Carbide Create imports DXF more happily than SVG, so take the DXF from this generator. Its coordinates are millimetres and its Y axis points up, matching the way Carbide Create thinks about a job.
The one thing you must get right on import is units. DXF R12 has no unit flag anyone should trust, so the dialog that asks you is not a formality.
Importing the DXF
Download the DXF and use File → Import in Carbide Create. When asked, choose millimetres. The file contains only LINE and ARC entities on a single layer, which is the most portable subset of the format.
After import you should see the pocket outline sitting in the first quadrant with an arc at each relieved corner, the same way round as the on-screen preview in the generator.
If the part looks flipped top to bottom relative to the web preview, you are looking at a different file or a third tool applied a Y flip. The DXF is not Y-flipped; the SVG is, because SVG's Y axis points down. Both describe the same physical part.
Creating the toolpath
Select the contour and create an inside or pocket toolpath with the same bit diameter you used in the generator. For a 1/4″ bit that is 0.25 in or 6.35 mm — pick one unit and use it in both places.
The contour already includes the dogbones, so a second offset by the radius is a mistake. Equally, a contour toolpath set to follow the line with no compensation will undersize the pocket by one radius and the tenon will not fit.
Set depth per pass for the material, not for the relief. A dogbone does not change the cutting load; it is the same pocket with a slightly longer perimeter.
You do not need boolean operations
A common workaround is to draw circles on the corners and boolean-union them into the rectangle. That is what this generator replaces.
The exporter rewrites each 90° corner directly into a line–arc–line sequence, so the file that reaches Carbide Create is already a single clean closed contour. You should not see overlapping circles sitting on top of a rectangle, and you should not need to union anything.
The practical benefit is that arcs stay exact. Boolean tools in drawing apps often polygonise curves, and a polygonised dogbone is a stack of tiny line segments that CAM has to re-fit.
Stock setup and depth
Set the stock thickness and zero before you judge anything on screen. Carbide Create draws the toolpath preview relative to stock top, and a wrong thickness makes a correct pocket look wrong.
Depth per pass is a material and cutter decision, unaffected by the reliefs. A dogbone adds a small amount of perimeter, not depth, so the cutting load per pass is essentially unchanged.
If you are pocketing through the material, remember that the relief arcs will also go through. On a through-pocket the dogbone becomes a visible notch on both faces, which is worth checking against the design before you cut.
Do not V-carve a relieved pocket
V-carve and advanced V-carve toolpaths compute their own corner behaviour from the shape outline. Feeding them a contour that already contains cutter-radius reliefs produces a corner that is relieved for one tool and carved for another.
Corner relief is only meaningful for an end mill of a known diameter. If the operation is a V-carve, generate the pocket without reliefs and let the V-bit reach the corner on its own — it can, because its tip radius is effectively zero.
When the export was refused
If an edge was too short for two reliefs, you never got a file — the generator reports which edge failed and by how much. Go back, disable one corner or switch to T-bone on auto, then re-export.
Do not scale the DXF in Carbide Create to make the dogbones fit. Scaling changes the whole pocket, and the relief radius has to stay equal to the cutter radius or the corner is not actually relieved.
Finish with a dry run above the stock. This site is independent and is not a Carbide 3D product; it just emits geometry their tools can mill.